The Designer's Guide Community Forum

The Designer's Guide Community Forum
https://designers-guide.org/forum/YaBB.pl
Simulators >> Circuit Simulators >> Any result browser can read spectre output?
https://designers-guide.org/forum/YaBB.pl?num=1224475924

Message started by john_ana on Oct 19^th, 2008, 9:12pm

Title: Any result browser can read spectre output?
Post by john_ana on Oct 19^th, 2008, 9:12pm

Greetings!

I am tired of debugging the bugs in cadence's wavescan. In my opinion, spectre is a very good
simulator but the back-end processing stuff such
as wavescan is kind of shaky and is not stable.
Sometime it works, sometime it doesn't. I am
looking for a robust result browser like awaves.
I know sandwork's SPICE explorer can read
the spectre's output and is very stable. However,
its license is kind of expensive. Any other tools
can read spectre's output directory?

I am wandering if there is a tool that can convert
spectre netlist to spice netlist. Usually foundry will
provide models for spectre and spice. If I can
get netlist in spicem, I can run Hspice and use
awaves to plot the results.

Thanks

Title: Re: Any result browser can read spectre output?
Post by Geoffrey_Coram on Oct 20^th, 2008, 6:19am

Sandwork was bought by Synopsys last year, I think; since you have other Synopsys tools, you might be able to get a decent price in a VPA for WaveView Analyzer (Spice explorer is something else).

You should also investigate the other output formats of Spectre -- maybe you can find one that your favorite viewer can read. (awaves is 2 generations old now; CosmoScope and now WaveView are the "newer" viewers)

Title: Re: Any result browser can read spectre output?
Post by Ken Kundert on Oct 20^th, 2008, 12:47pm

I believe that most people, when confronted with this problem, revert back to AWD.

-Ken

Title: Re: Any result browser can read spectre output?
Post by john_ana on Oct 20^th, 2008, 6:52pm

Ken and Geoffrey,

Thanks a lot for the reply. I am doing a TIA transient simulation and
I ran spectre in standalone mode (no GUI) After the simulation is
done, I use result browser or calculator to plot the output waveform
and do a FFT on the curve.

It is very weird that I can use calculator to plot the waveform, but
when I tried to use the dft function, it says something like:
("strcat" 43 t nil ("Error" strcat argument #1 should either be a
string or symbol ((type template = \"S\" nil))

The expression it calls error on is something like:
dft(v("/SO", ?resultDir "./simulation/test/spectre/schematic/psf" ?result "tran-tran") 20u 1m 65536 "Rectangular" 1 dftCoherentGain ("Rectangular",1))

I did some research on the output format, it seems I can use
options -rawfmt=nutbin,sst2,psfbin,wsfbin etc.

However to read nutbin results, do i need to have nutmeg installed?
any popular result viewer can handle this such as nWave? smartspice?

I also tried to use
simulator lang = spice
.fft V(SO) 20u 1m 65536

However it will report that the .fft card is not currently supported.

My question is how do I plot the fft without resorting to dump the
waveform into a text file? how to invoke AWD?

Title: Re: Any result browser can read spectre output?
Post by Geoffrey_Coram on Oct 21^st, 2008, 5:27am

nutmeg is the output format for Spice3 -- and there are other simulators (eg ADS and Spectre) that can be told to produce it; I've found some differences in their actual file format -- and, of course, some analysis types like PSS or HB that weren't in Spice3 may not have a nutmeg representation. I would think, though, that your transient analysis would work fine.

I found tools.lnx86/dfII/bin/awd in my Cadence install.

Title: Re: Any result browser can read spectre output?
Post by Frank Wiedmann on Oct 21^st, 2008, 6:11am

There have been a number of problems with the new sst2 format, so switching to psfbin might help you, see http://sourcelink.cadence.com/docs/db/kdb/2008/Feb/11422868.html.

Title: Re: Any result browser can read spectre output?
Post by jbdavid on Dec 18^th, 2008, 8:29pm

There is also a matlab code for reading psf data..

Title: Re: Any result browser can read spectre output?
Post by rf-design on Mar 4^th, 2009, 3:13am

Is that the cds2raw.m Matlab script which read psf data into matlab workspace?

I found it under the /spectre/matlab in the MMSIM dir.

Does it work with the default setting from a VADE?

Are there further docs beside the

matlabmeasug.pdf

*.pdf in the IC dir. It is not updated since 2004?

Title: Re: Any result browser can read spectre output?
Post by Andrew Beckett on Mar 4^th, 2009, 5:54am

Look in <MMSIMinstDir>/tools/spectre/examples/SpectreRF_workshop/SpectreRF_AN and you'll see MatlabWorkshop.pdf and MatlabAN.pdf which explain how to use it.

Broadly speaking though, you'll need this:

Code:

setenv MATLABPATH `cds_root spectre`/tools/spectre/matlab/64bit
setenv LD_LIBRARY_PATH `cds_root spectre`/tools/dfII/lib:`cds_root spectre`/tools/lib/64bit:$LD_LIBRARY_PATH

before launching matlab. The above settings are for if you're running 64 bit matlab; if 32 bit you'd omit the "/64bit" part from the MATLABPATH and LD_LIBRARY_PATH

This ensures that the MATLABPATH is set up OK, and the LD_LIBRARY_PATH contains
the right paths such that the toolbox can load its shared libraries.

The "cds_srr" command (part of the "Spectre Toolbox") can be used to
read all sorts of data from PSF - essentially you call it with:

cds_srr('/path/to/psf/dir'[,'datasetname'[,'signalName'])

and it returns:

1. With 1 arg - the datasets available (same as what you see in results
browser)
2. With 2 args - the signals in that dataset
3. With 3 args - the data for that signal. This may be a record with (say)
.V and .time elements, or it may be a matrix if there was some sweeps

The toolbox comes with a bunch of other higher level functions for plotting RF results - these are covered in the app note and workshop PDFs that I mention above.

You don't have to run spectre in any special way to be able to read the results - this reader can read PSF or SST2 simulation results.

Regards,

Andrew.