Designer’s Guide Community

Yutao Liu Community Member Offline Posts: 76 Guangzhou, China	how to simulate conversion gain from voltage noise to phase noise? Jan 11^th, 2010, 1:45am hi, everyone, it is reported that Spectre can simulate the conversion gain from voltage noise at any node of the circuit to phase noise? How should set up the simulation, since the circuit is autonomous? Thanks in advance!
Back to top	IP Logged

pancho_hideboo

Senior Fellow

Offline

Posts: 1424
Real Homeless

Re: how to simulate conversion gain from voltage noise to phase noise?
Reply #1 - Jan 11^th, 2010, 2:38am

Yutao Liu wrote on Jan 11^th, 2010, 1:45am:

How should set up the simulation, since the circuit is autonomous?

Even if your circuit is autonomous, set "Input Source" in Pnoise setting.
Here you have to put probe at location where you want to consider as input.

But I don't think such transfer function is useful.

Why don't you use PXF as slave analysis for master autonomous PSS analysis ?
Also in this case, you have to put probes at location where you want to consider as input.
Here you can treat multiple probes as input.

You had better restudy http://www.designers-guide.org/Forum/YaBB.pl?num=1260884939

PAC is SIMO(Single Input and Multiple Outputs) Analysis.
PXF is MISO(Multiple Inputs and Single Output) Analysis.

Back to top

« Last Edit: Jan 11^th, 2010, 4:55am 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

Andrew Beckett

Senior Fellow

Offline

Life, don't talk to
me about Life...

Posts: 1742
Bracknell, UK

Re: how to simulate conversion gain from voltage noise to phase noise?
Reply #2 - Jan 16^th, 2010, 8:35am

If you use spectre's PXF analysis with the option stimuli=nodes_and_terminals then it will compute the transfer function from every node and every terminal to the specified output. For nodes it is the transfer function from a current source connected to the node, and for terminals (device terminals) it is from a voltage source in series with the terminal.

Provided you've saved the node information and terminal information, you can get this - no need to add any additional components in the circuit. For node information you need to save "voltages", and for terminals you need to save "currents" (a bit misleading terminology because it's really the appropriate gain you're saving, but if you think of "voltages" as meaning "nodes" and "currents" as meaning "terminals", you're OK). So you may just want to save all node voltages and all device currents (on the Setup->Save Options form in ADE). Or of course you can just click on the terminals or nodes you want to save from Setup->Outputs to be Saved->Select on schematic

Regards,

Andrew.

Back to top

IP Logged