Designer’s Guide Community

john_ana

Junior Member

Offline

Posts: 12

Any result browser can read spectre output?
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

Back to top

IP Logged

Geoffrey_Coram

Senior Fellow

Offline

Posts: 1999
Massachusetts, USA

Re: Any result browser can read spectre output?
Reply #1 - 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)

Back to top

If at first you do succeed, STOP, raise your standards, and stop wasting your time.

IP Logged

Ken Kundert Global Moderator Offline Posts: 2386 Silicon Valley	Re: Any result browser can read spectre output? Reply #2 - Oct 20^th, 2008, 12:47pm I believe that most people, when confronted with this problem, revert back to AWD. -Ken
Back to top	IP Logged

john_ana

Junior Member

Offline

Posts: 12

Re: Any result browser can read spectre output?
Reply #3 - 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?

Back to top

IP Logged

Geoffrey_Coram

Senior Fellow

Offline

Posts: 1999
Massachusetts, USA

Re: Any result browser can read spectre output?
Reply #4 - 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.

Back to top

If at first you do succeed, STOP, raise your standards, and stop wasting your time.

IP Logged

Frank Wiedmann Community Fellow Offline Posts: 678 Munich, Germany	Re: Any result browser can read spectre output? Reply #5 - 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.
Back to top	IP Logged

jbdavid Community Fellow Offline Posts: 378 Silicon Valley	Re: Any result browser can read spectre output? Reply #6 - Dec 18^th, 2008, 8:29pm There is also a matlab code for reading psf data..
Back to top	jbdavid Mixed Signal Design Verification IP Logged

rf-design Senior Member Offline Reiner Franke Posts: 165 Germany	Re: Any result browser can read spectre output? Reply #7 - 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?
Back to top	IP Logged

Andrew Beckett

Senior Fellow

Offline

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

Posts: 1742
Bracknell, UK

Re: Any result browser can read spectre output?
Reply #8 - 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.

Back to top

IP Logged