Designer’s Guide Community

lunren

Community Member

Offline

Posts: 82
Asia

Switched capacitor circuit noise simulation
Oct 08^th, 2010, 12:41pm

Hi All,

I have a switched capacitor circuit which has three clock phases, ph1 and ph2 work at 25MHz and ph3 works at 50MHz. Clock is 3.3V pulse.

I am wondering if there is a way to use SpectreRF to run the pnoise or qpnoise?

My knowledge about pnoise is that PSS only works for the circuit which has only one tone; qpnoise is that QPSS only works for sinusoidal tone.

Thanks,

Back to top

Best Regards,

Lunren

IP Logged

lunren Community Member Offline Posts: 82 Asia	Re: Switched capacitor circuit noise simulation Reply #1 - Oct 8^th, 2010, 1:59pm I made the simulator to run with some tricks. Now I have another question. The clock in the circuit is 25MHz, but the circuit output is still at 50MHz, should I put 12.5Mhz or 25MHz in the Stop of pnoise form? Thanks,
Back to top	Best Regards, Lunren IP Logged

pancho_hideboo

Senior Fellow

Offline

Posts: 1424
Real Homeless

Re: Switched capacitor circuit noise simulation
Reply #2 - Oct 8^th, 2010, 10:55pm

I can't find out any measurement issue in your post.
Your question is no more than very easy usage of very specific vendor's simulator.

lunren wrote on Oct 8^th, 2010, 12:41pm:

My knowledge about pnoise is that PSS only works for the circuit which has only one tone;

Very completely wrong.

lunren wrote on Oct 8^th, 2010, 12:41pm:

qpnoise is that QPSS only works for sinusoidal tone.

Very completely wrong.

PSS is an expansion by single frequency basis while QPSS is an expansion by multiple frequency bases which have no common divisor frequency each other.

lunren wrote on Oct 8^th, 2010, 12:41pm:

I have a switched capacitor circuit which has three clock phases, ph1 and ph2 work at 25MHz and ph3 works at 50MHz.
Clock is 3.3V pulse.
I am wondering if there is a way to use SpectreRF to run the pnoise or qpnoise?

If you can understand PSS and QPSS correctly, such wondering never could arise.

In your case, fundamental frequency of PSS is 25MHz. And you can adopt PSS/Pnoise without any problem.
In your case, you can't use QPSS/QPnoise since 25MHz and 50MHz have common divisor frequency of 25MHz.

lunren wrote on Oct 8^th, 2010, 1:59pm:

The clock in the circuit is 25MHz, but the circuit output is still at 50MHz,
should I put 12.5Mhz or 25MHz in the Stop of pnoise form?

Are you mixing up "Pnoise(sources)" and "Pnoise(timedomain)", aren't you ?

Show me the reason why you want to include 12.5MHz as frequency for Pnoise analysis.

Generally I don't recommend to include fundamental frequency of master large signal steady state analysis as analysis frequency for slave small signal noise analysis.

See the followings.
http://www.designers-guide.org/Forum/YaBB.pl?num=1258339986/7#7
http://www.designers-guide.org/Forum/YaBB.pl?num=1258339986/13#13
http://www.designers-guide.org/Forum/YaBB.pl?num=1218622880/3#3

Back to top

« Last Edit: Oct 9^th, 2010, 4:19am by pancho_hideboo »

Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!!
http://www7.plala.or.jp/ungeromeppa/flash/kita.html
http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related

IP Logged

lunren

Community Member

Offline

Posts: 82
Asia

Re: Switched capacitor circuit noise simulation
Reply #3 - Oct 11^th, 2010, 12:47pm

pancho_hideboo wrote on Oct 8^th, 2010, 10:55pm:

I can't find out any measurement issue in your post.
Your question is no more than very easy usage of very specific vendor's simulator.

lunren wrote on Oct 8^th, 2010, 12:41pm:

My knowledge about pnoise is that PSS only works for the circuit which has only one tone;

Very completely wrong.

Thanks for reminding me. Almost forget how to use SpectreRF. PSS is used for one beat frequency and QPSS is used for more than one beat frequencies.

lunren wrote on Oct 8^th, 2010, 12:41pm:

qpnoise is that QPSS only works for sinusoidal tone.

Very completely wrong.

This is what I get from setting up the QPSS. The large signal can be pulse waveform, other medium signal must be sinusoidal waveform.

PSS is an expansion by single frequency basis while QPSS is an expansion by multiple frequency bases which have no common divisor frequency each other.

lunren wrote on Oct 8^th, 2010, 12:41pm:

I have a switched capacitor circuit which has three clock phases, ph1 and ph2 work at 25MHz and ph3 works at 50MHz.
Clock is 3.3V pulse.
I am wondering if there is a way to use SpectreRF to run the pnoise or qpnoise?

If you can understand PSS and QPSS correctly, such wondering never could arise.

In your case, fundamental frequency of PSS is 25MHz. And you can adopt PSS/Pnoise without any problem.
In your case, you can't use QPSS/QPnoise since 25MHz and 50MHz have common divisor frequency of 25MHz.

Right, PSS+Pnoise works great. Thanks for correcting me.

lunren wrote on Oct 8^th, 2010, 1:59pm:

The clock in the circuit is 25MHz, but the circuit output is still at 50MHz,
should I put 12.5Mhz or 25MHz in the Stop of pnoise form?

Are you mixing up "Pnoise(sources)" and "Pnoise(timedomain)", aren't you ?

Show me the reason why you want to include 12.5MHz as frequency for Pnoise analysis.

I know for Pnosie(source), the frequency range should be from 0 to inf and for Pnoise(timedomain), the frequency range should be from 0 to beat_frequence/2. I am using 12.5Mhz as the upper analysis frequency for Pnoise(timedomain).

Generally I don't recommend to include fundamental frequency of master large signal steady state analysis as analysis frequency for slave small signal noise analysis.

See the followings.
http://www.designers-guide.org/Forum/YaBB.pl?num=1258339986/7#7
http://www.designers-guide.org/Forum/YaBB.pl?num=1258339986/13#13
http://www.designers-guide.org/Forum/YaBB.pl?num=1218622880/3#3

Back to top

Best Regards,

Lunren

IP Logged

pancho_hideboo

Senior Fellow

Offline

Posts: 1424
Real Homeless

Re: Switched capacitor circuit noise simulation
Reply #4 - Oct 12^th, 2010, 4:51am

lunren wrote on Oct 11^th, 2010, 12:47pm:

Thanks for reminding me. Almost forget how to use SpectreRF.

You are still misunderstanding PSS and QPSS of Cadence Spectre.

lunren wrote on Oct 11^th, 2010, 12:47pm:

PSS is used for one beat frequency
and QPSS is used for more than one beat frequencies.

Wrong.

There is no concept of "beat frequency" in both PSS and QPSS of Cadence Spectre.
See the followings.
http://www.designers-guide.org/Forum/YaBB.pl?num=1232036048/4#4
http://www.designers-guide.org/Forum/YaBB.pl?num=1268969030/7#7

lunren wrote on Oct 11^th, 2010, 12:47pm:

pancho_hideboo wrote on Oct 8^th, 2010, 10:55pm:

lunren wrote on Oct 8^th, 2010, 12:41pm:

qpnoise is that QPSS only works for sinusoidal tone.

Very completely wrong.

This is what I get from setting up the QPSS.
The large signal can be pulse waveform, other medium signal must be sinusoidal waveform.

Wrong.

Other medium signals also can be pulse waveform.

However from practical point of view, if you use pulse wave as medium signal,
convergence of QPSS of Cadence Spectre is very very very bad.
This is very true especially for Shooting-Newton-QPSS.

lunren wrote on Oct 11^th, 2010, 12:47pm:

I know for Pnosie(source), the frequency range should be from 0 to inf
and for Pnoise(timedomain), the frequency range should be from 0 to beat_frequence/2.
I am using 12.5Mhz as the upper analysis frequency for Pnoise(timedomain).

Did you describe you are invoking "Pnoise(timedomain)" in your post ?

And it has to be "fundamental_frequency/2" not "beat_frequency/2".

The followings are general notes for you.

- Always describe correct tool's name and vendor's name which you use as tool or simulator.
- Don't do multiple posts which are same content.
- Don't request source code or behavioral model without any efforts.
- There are many simulators which have analyses called as PSS, PAC and Pnoise.
- Describe in detail and correctly with using correct terminologies.
- Warnigns are different from Errors.
- ADS is not name of simulator.
- There is no tool which name is Cadence.
- Don't use Direct Plot of Cadence ADE blindly without knowing definition.
- All gains in Direct Plot of Cadence ADE are "right", "true" and "practical" voltage gain.
- Don't mix up Simulation with Post Processing. They are completely different phase.
- MATLAB are different from Simulink.
- Learn measurements using actual instruments. Not "EDA Tool Play

Back to top

« Last Edit: Oct 12^th, 2010, 9:03am by pancho_hideboo »

Kita━━━━━━(ﾟ∀ﾟ)━━━━━━ !!!!!
http://www7.plala.or.jp/ungeromeppa/flash/kita.html
http://www.youtube.com/watch?v=mjIxGh55bMM&feature=related

IP Logged