The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> performance analysis in ADE
https://designers-guide.org/forum/YaBB.pl?num=1176276350

Message started by Pavel on Apr 11^th, 2007, 12:25am

Title: performance analysis in ADE
Post by Pavel on 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.

Title: Re: performance analysis in ADE
Post by Andrew Beckett on 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.

Title: Re: performance analysis in ADE
Post by Pavel on 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.

Title: Re: performance analysis in ADE
Post by Andrew Beckett on 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.

Title: Re: performance analysis in ADE
Post by Pavel on 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.

Title: Re: performance analysis in ADE
Post by Andrew Beckett on 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.

Title: Re: performance analysis in ADE
Post by Pavel on 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.

Title: Re: performance analysis in ADE
Post by Andrew Beckett on 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.

Title: Re: performance analysis in ADE
Post by Pavel on 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.

Title: Re: performance analysis in ADE
Post by Andrew Beckett on 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.

Title: Re: performance analysis in ADE
Post by Pavel on 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.

Title: Re: performance analysis in ADE
Post by Andrew Beckett on 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.

Title: Re: performance analysis in ADE
Post by Pavel on 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.

Title: Re: performance analysis in ADE
Post by Andrew Beckett on Apr 12^th, 2007, 1:33am

Yes.

Title: Re: performance analysis in ADE
Post by Pavel on 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

Title: Re: performance analysis in ADE
Post by Andrew Beckett on Apr 13^th, 2007, 6:37am

It is NOT a different document. See the attached image. It's purely because your help system is not properly configured that a self-reference to the document is not working.

Andrew.

Title: Re: performance analysis in ADE
Post by Pavel on Apr 16^th, 2007, 1:52am

Ok, thanks Andrew.