Designer’s Guide Community

Pavel

Senior Member

Offline

Posts: 174
Lausanne/Switzerland

performance analysis in ADE
Apr 11^th, 2007, 12:25am

Hello,

Is there some possibility to do in ADE Cadence some sort of performance analysis, like in Orcad Spice.
Under performance analysis I mean dependence of some circuit parameter (gain, phase margin, etc.) from some component parameter (polarisation current, supply, component values, etc.).

For example, after making parametric analysis in AC, where parameter is polaristaon current, how can I get a graph of a Gain at 1 Hz versus polarisation current.

I searched in Cadence manuals, but nothing found.

Regards,

Pavel.

Back to top

IP Logged

Andrew Beckett Senior Fellow Offline Life, don't talk to me about Life... Posts: 1742 Bracknell, UK	Re: performance analysis in ADE Reply #1 - Apr 11^th, 2007, 6:36am It sounds as if this might be spectre's "sens" analysis (which is a small-signal sensitivity analysis)? Andrew.
Back to top	IP Logged

Pavel Senior Member Offline Posts: 174 Lausanne/Switzerland	Re: performance analysis in ADE Reply #2 - Apr 11^th, 2007, 6:58am Thank for response Andrew From which tool can I get acces to this "sens" analysis to see if it's that what I mean? Regards. Pavel.
Back to top	IP Logged

Andrew Beckett Senior Fellow Offline Life, don't talk to me about Life... Posts: 1742 Bracknell, UK	Re: performance analysis in ADE Reply #3 - Apr 11^th, 2007, 7:05am Well, if you're using ADE, and have spectre as the simulator, sens will show up in the list of analyses. You might also want to read the documentation, via cdsdoc (or type "spectre -h sens" for a short help on the analysis. Andrew.
Back to top	IP Logged

Pavel

Senior Member

Offline

Posts: 174
Lausanne/Switzerland

Re: performance analysis in ADE
Reply #4 - Apr 11^th, 2007, 7:32am

Ok, I found it.

It's not realy what I need.
In Orcad Spice it's easily.
First I do parametric analysis (AC for instance), second click on buton "Performance analysis" (or something like that), and then choose in opened window some performance function (for instance Gain at 1Hz).

Result is graph, where x axe - parameter value, y axe - performance function.

Does similar procedure exist in Cadence ADE?

Regards.

Pavel.

Back to top

IP Logged

Andrew Beckett

Senior Fellow

Offline

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

Posts: 1742
Bracknell, UK

Re: performance analysis in ADE
Reply #5 - Apr 11^th, 2007, 7:35am

OK, I understand now. This is much simpler. You can either use the Direct Plot form to plot many things, or use the calculator to calculate a particular value. If the result of that calculation is a scalar value (e.g. phaseMargin, gain bandwidth, etc) then if you do a parametric sweep (Tools->Parametric Analysis) then it will plot that scalar value versus the swept parameter.

Regards,

Andrew.

Back to top

IP Logged

Pavel

Senior Member

Offline

Posts: 174
Lausanne/Switzerland

Re: performance analysis in ADE
Reply #6 - Apr 11^th, 2007, 7:58am

Maybe there is some misunderstanding, but I didn't get desired graph, but many courbes on the same graph.
My approach was as follows.

In ADE
1. Setup AC analysis F1 ... F2
2. Cnoose output to plot - out1.
3. Run AC simulation -> V(out1) vs. freq appeared in WaveScan window
In WaveScan
4. Using calculator transformed V(out1) vs. freq in dB20(V(out1)) vs. freq
In ADE
5. Tools-> Parametric Analysis setup parameter sweep and run simualtion
In WaveScan
6. Several graphs appered in the form: V(out1) vs. freq, but not dB20(V(out1)) vs. freq

Where I was wrong?

Regards.

Pavel.

Back to top

IP Logged

Andrew Beckett

Senior Fellow

Offline

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

Posts: 1742
Bracknell, UK

Re: performance analysis in ADE
Reply #7 - Apr 11^th, 2007, 8:01am

Pavel,

If you used the value() function to plot the amplitude at a particular frequency (say), it would then result in a scalar value - and so would be plotted against the swept variable. Or you could use the bandwidth calculator function to find the (say) 3dB bandwidth.

In your case the calculator result is a waveform (not a scalar) in the case of a single run, and so when doing a parametric sweep, it can't plot it against the swept variable. Instead, it plots a family of curves - one per point in the parametric sweep.

Regards,

Andrew.

Back to top

IP Logged

Pavel

Senior Member

Offline

Posts: 174
Lausanne/Switzerland

Re: performance analysis in ADE
Reply #8 - Apr 11^th, 2007, 8:25am

Now my approach was as follows:

In ADE
1. Setup AC analysis F1 ... F2
2. Cnoose output to plot - out1.
3. Run AC simulation -> V(out1) vs. freq appeared in WaveScan window

In WaveScan
4. Using calculator transformed V(out1) vs. freq in dB20(V(out1)) vs. freq
5. Using calculator value function calculated dB20(V(out1)) at frequency 1 Hz (correct value appeared in WaveScan)

In ADE
6. Tools-> Parametric Analysis setup parameter sweep and run simualtion

In WaveScan
7. The same as before - several graphs V(out1) vs. freq

Best Regards

Pavel.

Back to top

IP Logged

Andrew Beckett

Senior Fellow

Offline

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

Posts: 1742
Bracknell, UK

Re: performance analysis in ADE
Reply #9 - Apr 11^th, 2007, 10:44pm

That's because you're still plotting v(out), not the value at 1Hz.

If you use Outputs->To Be Plotted, it's going to just plot the whole waveform - and consequently a family of curves if you do a parametric analysis.

Instead, use Outputs->Setup, and click on the Open button (next to the calculator expression). Build the expression as before - which will be something like:

db20(value(VF("/out") 1))

and then hit the Get Expression button in the Setup Outputs form. Give it a name, mark it to be plotted, and then Add.

Now when the simulation has finished, it will auto plot the expression versus the swept value.

Alternatively, just build the expression in the calculator after the simulation, and hit the plot icon in the calculator - this will do the same thing.

It would be wise to spend some time reading the manual. Hit the Help button in the corner of the ADE window, or run "cdsdoc" from the UNIX window, or take a look at <instdir>/doc/anasimhelp/anasimhelp.pdf . These are very basic usage questions, and reading the documentation is a good place to start.

Regards,

Andrew.

Back to top

IP Logged

Pavel

Senior Member

Offline

Posts: 174
Lausanne/Switzerland

Re: performance analysis in ADE
Reply #10 - Apr 12^th, 2007, 12:24am

It works, thanks Andrew. :)

Two small questions:
1. Official titre of document you mentioned in your message (....anasimhelp.pdf). In my setup help isn't properly configured, so I have to download help docs from our internal technical support site.
2. In my version of calculator there is no plot icon (plese, see the picture).

Best Regards.

Pavel.

Back to top

calculator_window.jpg

IP Logged

Andrew Beckett Senior Fellow Offline Life, don't talk to me about Life... Posts: 1742 Bracknell, UK	Re: performance analysis in ADE Reply #11 - Apr 12^th, 2007, 1:12am Pavel, The little graph icon to the right of the Append cyclic, and above the Eval button is the "plot" icon I was referring to. This will plot whatever you have in the calculator buffer. Your first question wasn't really a question - so I'm not sure how you're expecting me to answer it? Regards, Andrew.
Back to top	IP Logged

Pavel Senior Member Offline Posts: 174 Lausanne/Switzerland	Re: performance analysis in ADE Reply #12 - Apr 12^th, 2007, 1:21am Andrew, I mean title of document that figures on 1st page. For example I have .pdf where on 1st page there is title Virtuoso� Analog Design Environment User Guide Is it the document what you mean? Regards, Pavel.
Back to top	IP Logged

Andrew Beckett Senior Fellow Offline Life, don't talk to me about Life... Posts: 1742 Bracknell, UK	Re: performance analysis in ADE Reply #13 - Apr 12^th, 2007, 1:33am Yes.
Back to top	IP Logged

Pavel Senior Member Offline Posts: 174 Lausanne/Switzerland	Re: performance analysis in ADE Reply #14 - Apr 12^th, 2007, 2:39am Andrew, I just worked with Virtuoso� Analog Design Environment User Guide. There I clicked on a link that readressed me to anasimhelp.pdf. As in my environment help isn't properly installed, system couldn't find it. But one thing is clear - anasimhelp.pdf is some other document. Regards, Pavel
Back to top	IP Logged