APS:Monte Carlo:Output waveforms in a single file

Ionut,

It does - it builds a family of curves (a "single waveform" wouldn't make sense, but you can have a family of curves, so you can open a single database which gives you all of the results across the run, assuming that you've saved family data using the savefamilyplots=yes option to the montecarlo analysis). If you're using the export=oceanEval(...) type syntax to generate scalar measurements from each point, you can use the abMonteWaveform function in the abStats.il code attached to solution 11026072.

Regards,

Andrew.

  Hi Andrew,

 Thank U for the response... I have added the option in my spice deck (spice format), but the tool still dumps multiple waveform files for each Monte Carlo and no general file that contains all of the data. Below is the syntax I have used within spice deck:

simulator lang=spectre
simulatorOptions options savefamilyplots=yes
simulator lang=spice

 Below is the command line:

    aps +spice aps.sp +escchars +log aps.log -format wdf -raw ./psf +aps=conservative +mt=1 +lqtimeout 0

 Regards,

Ionut

Hi Ionut,

It's an analysis option, not a global option, so it would need to go on the monte carlo analysis statement.

Before showing how to do that, it would be far more helpful to understand how you have the analysis statements defined right now in your netlist - because there are several ways of defining a monte carlo analysis. So can you show the analysis/options statements in the netlist that you have right now?

Kind Regards,

Andrew.

  Hi Andrew,

  Below is the transient analysis setting that I am using for running monte carlo:

* TRAN analysis
**********************************************************************************
.param xlnx_tran_step   = 1ns

.param xlnx_tran_stop   = 100ns

.tran xlnx_tran_step xlnx_tran_stop SWEEP MONTE=5
 

 Regards,

Ionut

Hi Ionut,

I just tried using this, and it already saves the family data. I used the statements you provided above, and I get this:

UNIX> ls monteres.raw
logFile      sweep1-001_timeSweep.tran  sweep1-003_timeSweep.tran  sweep1-005_timeSweep.tran
logFile.tmp  sweep1-002_timeSweep.tran  sweep1-004_timeSweep.tran  sweep1_timeSweep.montecarlo

The last file is the root of the tree to give a family of the individual iteration results. If I open this result directory in ViVA, I see the picture in the attachment below. As you can see, I see "tran" as the results, and the set of waveforms gets opened together.

What tool are you using to look at the waveforms? 

The alternative would be to use spectre syntax for the monte carlo, but that seems unnecessary here since it works fine:

simulator lang=spectre
parameters  xnlx_tran_stop=100n
monte montecarlo numruns=5 savefamilyplots=yes {
  tran tran stop=xnlx_tran_stop
}

there's no real need to set step= on the transient (you could if you really wanted to).

Kind Regards,

Andrew.

 Hi Andrew,

 I tried using the same syntax in my spice deck and below are the files generated:

transient1-000_transient1.tran  transient1-001_transient1.tran  transient1-002_transient1.tran  transient1-003_transient1.tran  transient1-004_transient1.tran  transient1-005_transient1.tran transient1.montecarlo

 

 The file that probably looks more like the one U mentioned is "transient1.montecarlo", but it does not seem to contain the proper data if loading it using CustomExplorer... I wonder if its the viewer I'm usin ?:(

 Regards,

Ionut

Ionut,

I didn't notice the command line you were using earlier:

    aps +spice aps.sp +escchars +log aps.log -format wdf -raw ./psf +aps=conservative +mt=1 +lqtimeout 0

You're using WDF as the output format. There's only limited support for WDF in the advanced analyses, and so whilst it writes the individual transient results in WDF format, the "collection" database (transient1.montecarlo in your case) is written in PSF still (not sure if WDF has a way to describe things in the same way).

If you were to write out using psfxl as the format, and then use "viva" to plot the results, you wouldn't have this limitation. That's the primary use model - write the results from a Cadence simulator in a Cadence format and view using a Cadence waveform viewer... 

Kind Regards,

Andrew.